5ax curve from plane

[LucasGC]

Hi all,

I've made a few 3ax toolpaths with the 5ax curve toolpath by just setting my axis control to top plane and having zero lead/side tilt but still leaving it as 5-ax

Whenever my tool goes through this path it's staying straight up and down but the c-axis keeps rotating.

I'm just wondering what geometry in mastercam is telling the tool to rotate?

It's not a problem that it's rotating, I'm just wondering what's going on 'behind the scenes'

[LucasGC]

Actually ran into a somewhat example.

Have a 5-ax multisurf op that really only needs to tilt b and not rotate during cut. 

I'm seeing it unwind right after it begins the cut, i think what's happening is it's plunging at c180, and then once it gets to the first cut point it rotates c270, and the next point is c360, which my machine should be able to get to, but it unwinds to c180 and stays there for the rest of the cuts.

Just trying to find out what's making it rotate! Thanks

OP 4 5ax multisurf

 

G90
G00 X9.6595 Y13.6673 Z12. C0. B0. (PZN2O SB)
G00 Z6.
G00 X9.6593 Z2.1 C180.
G01 Z2. C270. F100.
G01 Y13.6624 F200.
G01 Y2.2104 C358.8749
(*** Reposition ***)
(*** Vertical to Angle On A, B Axis ***)
(***  Retract Length : 3.   ***)
G01 X9.6595 Y2.2104 Z5. F2100.
G00 Z12. (Move Z TC Height - P_UNWIND SB)
G00 X10.1733 Y2.2031 C180. B-2.7108
G00 Z4.9878
G01 X9.6593 Y2.2104 Z2. (Back to Previous Position)
F200. (Reset Feed Rate)
(*** End Reposition ***)
G01 X10.0314 Y2.2031 Z1.9912
G01 Y2.2053

seat cushion core aft seat bottom.mcam

[Colin Gilchrist]

Whenever you have 5-Axis output, those moves are "Vector-based". Internally, in the Post Processor, anytime you have a Tool Vector that approaches "vertical", where your Primary Axis of rotation is perpendicular to that "Vertical Tool Vector", you have what is known as a "singularity". This is where there are "infinite" possible C-Axis Positions, because mathematically, any C-Axis position is valid with a Vertical Tool Vector. Simple solution is to not use Curve-5X with a Vertical Tool, and only use it when you have a need to tilt the tool vector. Otherwise, the Post doesn't know that you're intending this to be a "locked C-Axis" path.

If you are using the Generic Fanuc 5X Mill Post (or a derivative of that Post, like the VF_TR Post), then there is really nothing you can do to prevent this.

[LucasGC]

11 minutes ago, Colin Gilchrist said:

Whenever you have 5-Axis output, those moves are "Vector-based". Internally, in the Post Processor, anytime you have a Tool Vector that approaches "vertical", where your Primary Axis of rotation is perpendicular to that "Vertical Tool Vector", you have what is known as a "singularity". This is where there are "infinite" possible C-Axis Positions, because mathematically, any C-Axis position is valid with a Vertical Tool Vector. Simple solution is to not use Curve-5X with a Vertical Tool, and only use it when you have a need to tilt the tool vector. Otherwise, the Post doesn't know that you're intending this to be a "locked C-Axis" path.

If you are using the Generic Fanuc 5X Mill Post (or a derivative of that Post, like the VF_TR Post), then there is really nothing you can do to prevent this.

Interesting, so it's just free to do what it wants. Well it makes sense, but for the last toolpath i posted it seems like i'm out of luck. The first cut is vertical and i can't get the unwind out of it

[Colin Gilchrist]

2 minutes ago, LucasGC said:

Interesting, so it's just free to do what it wants. Well it makes sense, but for the last toolpath i posted it seems like i'm out of luck. The first cut is vertical and i can't get the unwind out of it

Since the 5X Post is 'Generic' in nature, CNC Software set it up with a bunch of "controls", in the form of 'miscellaneous integers and real numbers' these act as 'switches' to the Post, and give you control over certain aspects of the posting process.

Try setting 'mi4$' to either +180, or -180, and see if that avoids the unwind move.

On machines like a Gantry Mill, with limited C-Axis (Primary) motion, you can "prewind" the head with Mi4 and/or MI5.

Also, try setting MI10 to '1' or '2' to restrict the Secondary Travel Range. Sometimes this can be used to trick the Post.

What machine is this, and what are your Rotary Limits for Primary and Secondary?